[Gmsh] meshing partitions

Fri May 15 15:04:05 CEST 2020

Hello,
Thanks a lot for the support. Meshing in two steps and noting the
NbNodes and elements (NbTriangles, Nbquads) worked. I get a correct
mesh in gmsh and also saving the result is correct.
I still have some problems importing the final BDF mesh into ansys
fluent (gmsh reads and displays the BDF correctly)

The BDF contains the diagonal edges twice although I use Coherence Mesh.

after deleting
CBAR    1 ...
...
CBAR   16 ...

by hand I can read the combined BDF mesh into ansys.

I attached all three sample geo files for all three steps (mesh_1.geo,
mesh_2.geo and mesh_combined.geo) for reference

Thanks a lot again.

Cheers,
hj

On Mon, May 11, 2020 at 5:30 PM Christophe Geuzaine <cgeuzaine at uliege.be> wrote:
>
>
>
> > On 11 May 2020, at 16:32, Hansjoerg Seybold <hansjoerg at fisica.ufc.br> wrote:
> >
> > Hello,
> > Thanks a lot for the reply. Using the visibility filter worked. I
> > created a simple test case (attached)
> > which creates the two mesh pieces. So now I have two meshes
> > multizone_1.msh and multizone_2.msh
> > which I can load in a geo file
> > --------------------------------------
> > Merge "multizone_1.msh";
> > Merge "multizone_2.msh";
> > Coherence Mesh;
> > Save "multizone_merged.msh";
> > Save "multizone_merged.bdf";
> > Exit;
> > --------------------------------------
> > I understood that the coherence mesh removes the duplicate nodes on
> > the common edge and the above
> > script displays the mesh in the gui correctly.
> > However the export is distorted as the node ordering is not updated.
> > I would get the development snapshot to try to use the mesh tag
> > suggestion, but how would I do the reordering
> > starting from the script above?
> >
>
> You would do:
>
> Mesh.FirstNodeTag=1;
> Mesh 2;
> Save "multizone_1.msh";
>
> ...
>
> Mesh.FirstNodeTag=Mesh.NbNodes + 1;
> Mesh 2;
> Save "multizone_2.msh";
>
>
> > regarding openmp:
> >
> > We (the IT cluster staff at ETH Zurich and myself) tried to get the
> > openmp version of gmsh running on the cluster (CentOS 6), but without
> > success.
> > I managed to compile and run it on my ubuntu PC, but with very little
> > speedup for the selected meshing algorithm.
> > I tested openmp with two physical groups active and -nt 2, on a finer
> > LC as in the attached geo for speed measurements and Mesh.Algorithm =
> > 9; gmsh-4.4.1,
> > a significant speedup could only be observed for del2d, but quality
> > tests showed that the 'pack' algorithm gave the best meshing result
>
> Ok I see. The "pack" algorithm has not been worked on for a while and is indeed currently sequential. We are working on updating this algorithm, so hopefully it will get much faster (and parallel) soon.
>
> > BTW, is it possible to apply different meshing algorithms to different
> > physical groups?
> >
>
> Yes. In .geo files: MeshAlgorithm Surface {...} = ...;
>
> Christophe
>
>
> > Regarding the 5 days meshing: I am using quad meshing (algo 9) with a
> > not too sophisticated sizing function but with a very large domain,
> > del2d is orders
> > of magnitudes faster.
> >
> > Thanks a lot for the help.
> >
> > Hansjoerg
> >
> >
> >
> >
> >
> >
> >
> > On Sun, May 10, 2020 at 9:05 AM Christophe Geuzaine <cgeuzaine at uliege.be> wrote:
> >>
> >>
> >>
> >>> On 9 May 2020, at 18:09, Hansjoerg Seybold <hansjoerg at fisica.ufc.br> wrote:
> >>>
> >>> Hello,
> >>> I am trying to mesh a model consisting of several physical groups each
> >>> group at a time and then merge the meshes for the different physical
> >>> groups afterwards. The reason why I am trying to perform this "domain
> >>> decomposition" is that the meshing of the full model takes over 5 days
> >>> and exceeds the runtime limit of the queuing system.
> >>>
> >>> However I could not find a simple way to apply the  "Mesh 2" to a
> >>> specific physical group. Gmsh always tries to mesh the whole model.
> >>>
> >>
> >> You could either delete the parts you don't want to mesh; or hide the parts you don't want to mesh (cf. the `Show` and `Hide` commands in .geo script, or `setVisibility()` in the api) and use the `Mesh.MeshOnlyVisible` option.
> >>
> >>> My question would be if anybody has a hint how to perform this meshing
> >>> in parts and how to combine the resulting meshes into a single final
> >>> model.
> >>>
> >>
> >> That's trickier as each mesh will be independent. The development snapshot allows you to set the starting node/element tag (Mesh.FirstNodeTag, Mesh.FirstElementTag), which will help. Removing duplicate nodes when you merge things together can be done with Coherence Mesh (in .geo files) or removeDuplicateNodes() in the api.
> >>
> >> PS: 5 days to perform a 2D mesh ? Anything special in the geometry/size field? If you don't do this already at least recompile Gmsh with OpenMP enabled, and mesh in parallel?
> >>
> >> Christophe
> >>
> >>> Thank you very much.
> >>>
> >>> Best,
> >>> hansjoerg
> >>>
> >>> _______________________________________________
> >>> gmsh mailing list
> >>> gmsh at onelab.info
> >>> http://onelab.info/mailman/listinfo/gmsh
> >>
> >> —
> >> Prof. Christophe Geuzaine
> >> University of Liege, Electrical Engineering and Computer Science
> >> http://www.montefiore.ulg.ac.be/~geuzaine
> >>
> >>
> >>
> > <multizone_1.geo>_______________________________________________
> > gmsh mailing list
> > gmsh at onelab.info
> > http://onelab.info/mailman/listinfo/gmsh
>
> —
> Prof. Christophe Geuzaine
> University of Liege, Electrical Engineering and Computer Science
> http://www.montefiore.ulg.ac.be/~geuzaine
>
>
>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: mesh_1.geo
Type: application/octet-stream
Size: 1150 bytes
Desc: not available
URL: <http://onelab.info/pipermail/gmsh/attachments/20200515/c95902cc/attachment.geo>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: mesh_2.geo
Type: application/octet-stream
Size: 1184 bytes
Desc: not available
URL: <http://onelab.info/pipermail/gmsh/attachments/20200515/c95902cc/attachment-0001.geo>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: mesh_combined.geo
Type: application/octet-stream
Size: 113 bytes
Desc: not available
URL: <http://onelab.info/pipermail/gmsh/attachments/20200515/c95902cc/attachment-0002.geo>